What is CNC Cutting?

CNC (Computer Numerical Control) cutting is a subtractive manufacturing process that uses computer controlled tools to remove material from a piece of stock. A CNC router uses physical cutting tools that rotate at high speeds and move along programmed toolpaths.

CNC cutting can be used for a wide range of applications, from cutting flat parts out of sheet material to machining complex three-dimensional surfaces.

Understanding the available cutting tools, control geometry, common machining operations, and basic limitations of the CNC process is important when designing and preparing a project.

---

Cutting Tools

The CNC router uses interchangeable cutting tools designed for different types of machining. The diameter and geometry of the selected tool affect the type of cut that can be produced, the level of detail possible, and the resulting surface finish.

Square End Mills

Square end mills have a flat cutting end and are among the most commonly used CNC tools. They are well suited for profiling, pocketing, slotting, and horizontal roughing where a flat-bottomed cut is desired.

Larger diameter end mills can remove material more efficiently but cannot reproduce the same level of detail or tight inside corners as smaller diameter tools.

Ball End Mills

Ball end mills have a rounded cutting end and are primarily used for machining three-dimensional surfaces. They are commonly used for parallel finishing where the tool must follow changes in surface geometry.

Ball end mills are especially useful for topography, terrain, ramps, curved forms, and other contoured geometry. Smaller diameter ball end mills can reproduce finer surface detail but generally require more machining time.

Compression Bits

Compression bits combine up-cut and down-cut flute geometry to reduce chipping and tear-out on both the top and bottom faces of sheet material. They are primarily used for profiling sheet goods where a clean finished edge is important.

Compression bits are most effective when the cutting depth allows both portions of the flute geometry to engage the material.

Vee Mills

Vee mills have an angled cutting profile and are primarily used for engraving. They can be used for lettering, graphics, reference markings, and decorative surface details.

Because the width of the cut changes with depth, vee mills can produce fine lines near the tip and progressively wider cuts as the tool moves deeper into the material.

Drill Bits

Drill bits are designed specifically for drilling operations and create vertical holes at programmed locations.

---

Tool Library

The CNC router is equipped with an automatic tool changer. Seven standard tools are normally loaded in the machine, with one additional tool position available as needed. The standard tool library is designed to support a wide range of common CNC machining operations.

The maximum cut depth represents the approximate usable cutting depth of each tool. Project geometry, workholding, tool clearance, and machining strategy may further limit the depth that can be safely machined.

---

Control Geometry

RhinoCAM uses control geometry to define where a machining operation is applied. Depending on the operation, control geometry may include curves, closed boundaries, surfaces, or other model geometry.

Clean, well organized control geometry makes toolpath programming easier and helps limit machining to the intended areas of the model. Geometry should be checked for duplicate curves, gaps, overlaps, and other issues before programming the toolpaths.

---

Common CNC Operations

A CNC cutting project may use one or several machining operations, depending on the geometry and how the project needs to be fabricated. The type of operations, the number required, and the order in which they are performed are unique to each project.

Think of these operations as a sequence of fabrication steps, similar to planning how a project would be made in a traditional shop. Each operation performs a specific task, and together they form the machining strategy used to produce the finished project.

2½ Axis Profiling

Profiling follows selected control geometry and offsets the cutting tool to the appropriate side of the geometry. For closed boundaries, the tool can be positioned to the inside or outside so the finished part maintains the intended dimensions.

Profiling is commonly used to cut individual parts from a larger piece of stock or to cut the outside boundary of a model base.

2½ Axis Pocketing

Pocketing removes material from inside a closed boundary to a specified depth.

Pocketing is commonly used to create recesses, joinery, stepped changes in elevation, and other features with defined depths.

2½ Axis Engraving

Engraving follows selected curves to create lines or markings in the surface of the material. Unlike profiling, the tool generally follows the selected geometry directly rather than being offset to one side.

Engraving is commonly used for text, graphics, reference lines, roads, property lines, grids, and other surface information.

2½ Axis Drilling

Drilling creates vertical holes at specified locations. It is commonly used for fastener holes, alignment holes, and holes used to locate workpiece hold-down screws.

3 Axis Horizontal Roughing

Horizontal Roughing removes the majority of excess material required to produce a three-dimensional form by machining the stock in a series of horizontal layers.

A small amount of material is typically left for a subsequent finishing operation. Horizontal Roughing can also be used to create stepped or contour-style terrain by machining the geometry at a series of horizontal elevations.

3 Axis Parallel Finishing

Parallel Finishing uses closely spaced, parallel toolpaths that follow the three-dimensional surface of the model. It is commonly used after Horizontal Roughing to produce the final surface of terrain, ramps, curved forms, and other contoured geometry.

Ball end mills are commonly used for Parallel Finishing. Smaller stepovers generally produce smoother surfaces but require additional tool passes and increase machining time.

---

Tool Diameter & Inside Corners

Because CNC cutting tools have a physical diameter, an end mill cannot produce an inside corner that is sharper than the radius of the selected tool.

For example, a 1/4 inch diameter end mill has a 1/8 inch radius and will leave that radius at an inside corner.

This limitation is particularly important when designing joints, slots, pockets, and components that must fit together. Features such as dog bone or T bone fillets may be used when a square component must fit into an inside corner.

Smaller tools can produce tighter corners and finer details but generally remove material more slowly and may be more susceptible to breakage. Tool diameter and cutting length should therefore be considered when designing small or deep features.

---

Stepdown & Stepover

CNC tools generally remove material incrementally rather than cutting to the final depth or surface in a single pass.

Stepdown controls the vertical distance between successive cutting levels. A deeper operation may require several stepdowns before reaching its final depth.

Stepover controls the lateral distance between adjacent tool passes. Smaller stepovers generally produce a finer surface finish but require more passes and increase machining time.

The appropriate stepdown and stepover depend on the cutting tool, material, machining operation, desired surface quality, and other cutting parameters.

---

Feeds & Speeds

Feed rate describes how quickly the cutting tool moves through the material, while spindle speed describes how quickly the tool rotates.

Feed rate and spindle speed work together with the cutting tool geometry and number of flutes to determine how much material is removed as each cutting edge passes through the stock.

The Digital Fabrication Lab’s RhinoCAM PDF Guide provides appropriate parameters for the tools and materials commonly used in the lab.

Incorrect feed rate or spindle speed can result in poor cut quality, excessive heat, premature tool wear, or tool failure.

---

Workholding

Material and finished parts must remain securely held throughout the entire machining process. The appropriate workholding method depends on the material, stock dimensions, and machining operations being performed.

When arranging parts, leave sufficient material around and between components for workholding, tool clearance, and tabs. Sheet goods generally require additional material around the perimeter so the stock can be secured without interfering with the toolpaths.

The machining sequence should also account for how individual parts will remain secured after they are separated from the surrounding stock. A loose part can move into the cutting tool, creating a safety hazard and potentially damaging the project or equipment.

Bridging Tabs

Bridging tabs leave small portions of material connecting a finished part to the surrounding stock. These connections prevent the part from moving after the profile operation has cut around it.

Tabs are removed after machining, and the remaining material can be trimmed or sanded flush.

Onion Skinning

Onion skinning leaves a thin layer of material at the bottom of a profile rather than cutting completely through the stock. The remaining layer holds the parts in place during machining and is removed afterward.

This technique works best with flat, consistent material and may be less reliable with warped or lower-quality sheet goods.

Remove remaining tabs or onion skin carefully by sanding, trimming, or using a router with a flush-trim bit. Avoid breaking parts away by hand, particularly with veneered sheet goods, because this can tear or chip the finished surface.